Group Actions
Engagement
  • Author Author: camuyano
  • Date Created: Date Created
  • Views 2398 views
  • Likes 2 likes
  • Comments 8 comments
Related
Recommended

New parts, new part PCB Problem

camuyano

I had a wake up call using Eagle Cad and a third party libraries. And I wanted to share how my ignorance caused my boards to fail (for now).

Just for reference the board uses an Atmega328P SMD and i wanted a smaller and cheaper part than a normal crystal. So I went with a resonator, there are a few very cheap and very small. I am not that good on creating parts layout by myself so I searched on the libraries at hand for a resonator with the footprint similar to the one I wanted to use. And very quickly I found a smd resonator on Sparkfun-FreqCtrl library and the part is RESONATOR-SMD. First I was very happy to actually found this part. So I put the part on my PCB and send it to fab for manufacturing. The board came back beautiful red (I had to pay a little more for color selection). Then I notice that around the resonator there were some solder mask missing, but said to myself this must be a size limitation from that cheap Chinese fab. I am like a little kid whenever I get mail, so I ran to get my iron and started soldering. "No need to do any measurement, I am 99.9% sure the design is correct" I said. If fail then I will test, but I wanted to solder right away. So I did.

Latter after the boards start failing I then went back and did some measurement, just to find some missing solder mask and some exposed copper. The copper exposed then again I thought at first it was because of Chinese fab, but turn to be my mistake not the fab.

Lets see the picture bellow, look the black region is missing red solder mask. And at the borders you can see exposed copper (blue arrows). The missing solder mask (black part) does not causes any problem. However the exposed copper do. It causes my resonator to short to ground making my board fail.

image

 

And what was the cause of all? The actual part on the library had instructions to be constructed exactly as it was done. There is a layer in eagle called tStop. The tStop layer is the one that allows solder areas of copper to be exposed. This layer stops solder mask in a specific area. This part has a rectangle over the entire part. The size of this rectangle plus a small isolation in the board causes this tStop rectangle to go over my ground plane, and causes the copper to be exposed. On the image bellow, the big white hatched rectangle is the tStop that caused the problem. This made my twenty boards order to fail.

image

 

I have three options:

1. Etch (manually)  out that exposed copper to a distance that I can solder the part

2  Cover with heat resistant tape the exposed copper

3. Paint it over with solder mask (that I do not have at hand).

I am going to get a few pieces of tape, and try to cover the exposed copper in order for me to use these boards. But anyhow I edited my design and send a few more to be made, this project need to be finished and quickly. In about two weeks I should be getting them back and hope this issue is water under the bridge.

 

Hardware design has its ups and down, but it is well worth it. You win some and loose some and learn a lot during the process.

I should try to contact SparkFun about the part, or submit a pull request with the fix. I am a noob, this might be the right design and I am the one mistaken. Anyhow for PCB with a big ground plane close to this part this is not working. My guess is that the rectangle is intended to avoid ground plane under the part and not to stop the solder mask. This must be a layer mistake.

 

For the new PCB I did a ground plane cutoff polygon around the resonator, removed the tStop from the part and made the side contacts a little bigger (for easier soldering). When I get the PCB back from fab will post again with the new board. Hope that it work.

 

This PCB eagle files are not posted now, because this board is for a surprise event. After the event all will be posted. If you want to know, the board is just a usbaspLoader using an Atmega328P with an Arduino header footprint. Nothing revolutionary. Oh and of course, instead of a crystal with two capacitors it is using a 16Mhz resonator.

Parents

  • Just submitted a pull request on github to have this part fixed on the library. Soon should know if it is accepted. Just to avoid this from happening to others.

  • in reply to camuyano

    Hi Javier,

    We are really sorry to hear you had this problem with your boards. Thanks for posting about this and we appreciate your efforts to fix it in the library!

     

    As you have come to see (and it never stops, we're all still learning), Eagle is full of easy ways to make mistakes. Unfortunately, the smallest mistakes are often the most troubling (and sometimes detrimental to the design).

     

    We have used this current footprint for years, and it hasn't exposed the nearby pour on our designs because we always have our isolate on our pours set to 12 mil.

     

    image

     

    Here is a screen shot of the "Top" and "tstop" layers on our Arduino Pro Mini.


    image

    As you can see, the copper pour is just far enough that is not exposed. And on this particular layout, the bottom side doesn't even have space for the pour to flow. Looking at this now, I do see that there is a slight overlap on the top side of the crystal, and so I agree that this footprint could be improved. Perhaps we could add in some trestrict to inhibit any pour from going under the resonator mask.

     

    For your reference, you can download the full eagle files of the Arduino Pro Mini 328 here: https://github.com/sparkfun/Arduino_Pro_Mini_328

     

    Also, in case you are interested, we originally added in the "tstop" rectangle to intentionally remove the mask beyond the ends of the part. One thing we have found with our PCB fab house (and is the case with most), is that the mask layer is often not perfectly aligned with the copper. Sometimes it can be as far as 3 or 4 mil off. This is why most footprints actually include a buffer and the "tstop" is larger than the copper landing. This is done to ensure that 100% of your pad is exposed. So to help avoid this problem entirely, we just removed all the mask under (and around) the crystal.

     

    A second reason, and perhaps the more important one, is that mask can create an un-even surface below your part, where as the fiberglass is almost always perfectly flat. So with the mask removed, we are more likely to have a perfectly smooth surface underneath the part. This way the part can rest nicely on the solder paste during reflow and not be help up by any imperfections in the mask.

     

    Hope this helps and thanks again!

    -Pete Lewis (QC Manager at SparkFun)

Comment
  • in reply to camuyano

    Hi Javier,

    We are really sorry to hear you had this problem with your boards. Thanks for posting about this and we appreciate your efforts to fix it in the library!

     

    As you have come to see (and it never stops, we're all still learning), Eagle is full of easy ways to make mistakes. Unfortunately, the smallest mistakes are often the most troubling (and sometimes detrimental to the design).

     

    We have used this current footprint for years, and it hasn't exposed the nearby pour on our designs because we always have our isolate on our pours set to 12 mil.

     

    image

     

    Here is a screen shot of the "Top" and "tstop" layers on our Arduino Pro Mini.


    image

    As you can see, the copper pour is just far enough that is not exposed. And on this particular layout, the bottom side doesn't even have space for the pour to flow. Looking at this now, I do see that there is a slight overlap on the top side of the crystal, and so I agree that this footprint could be improved. Perhaps we could add in some trestrict to inhibit any pour from going under the resonator mask.

     

    For your reference, you can download the full eagle files of the Arduino Pro Mini 328 here: https://github.com/sparkfun/Arduino_Pro_Mini_328

     

    Also, in case you are interested, we originally added in the "tstop" rectangle to intentionally remove the mask beyond the ends of the part. One thing we have found with our PCB fab house (and is the case with most), is that the mask layer is often not perfectly aligned with the copper. Sometimes it can be as far as 3 or 4 mil off. This is why most footprints actually include a buffer and the "tstop" is larger than the copper landing. This is done to ensure that 100% of your pad is exposed. So to help avoid this problem entirely, we just removed all the mask under (and around) the crystal.

     

    A second reason, and perhaps the more important one, is that mask can create an un-even surface below your part, where as the fiberglass is almost always perfectly flat. So with the mask removed, we are more likely to have a perfectly smooth surface underneath the part. This way the part can rest nicely on the solder paste during reflow and not be help up by any imperfections in the mask.

     

    Hope this helps and thanks again!

    -Pete Lewis (QC Manager at SparkFun)

Children
  • in reply to Former Member

    First, thanks for the response. This is a pretty well explanation of the part and it make sense why the part is like that. Actually I think I will take back the pull request.

    I read from several places (I think it was dangerous prototypes) about the isolation. So I'm using 0.016 to be on the safe side and still it happened. But my boards are being made in the cheapest china service I could find, so these are not like production quality.

    Since I remove my tStop rectangle, I hope the solder mask size don't mess up my alignment. I am soldering this by hand so it might not be so bad a little offset in my case.

     

    This board was my mistake and somehow I am happy that it happened, I learn more from mistakes than for successes. And to top that, your explanation. Again, thanks for the  comment and now I can understand why the part was like it is.

    What you guys do at Sparkfun is really great, I am using your libraries, schematics and videos as my learning tools. Specially from your According to Pete videos.

     

    Question:

    The picture above of the part, is from an actual design and it does not exposes a bit of the top copper plate? The tStop looks pretty close on the top side, the bottom side has more than enough space.

     

    Again thanks for the response, I didn't expect so good feedback. If you ever come down to Puerto Rico, your first Pina Colada is on me.

  • in reply to camuyano

    Javier, You are very welcome! We are always happy to help. And we are glad that you see your mistake as learning experience - that's a great outlook on life in general!

    The picture above of the part, is from an actual design and it does not exposes a bit of the top copper plate?

    You are right, according to the eagle file, it does look like a tiny sliver of copper would be exposed. Looking at a physical board with a monocle, I can see that the mask actually ends up covering up the ground pour and extending over about 2 or 3 mil. I suppose this is just because mask is like silk screening and it starts as a liquid of sorts. And so there will always be the slightest amount of bleed.

     

    Regardless, I do think that is is bad practice to have this overlap in the package, so I have adjusted our library to include some tRestrict.

     

    image

    Just commited it to our library, so you can see it in eagle if you like. These tRestrict rectangles will cause any polygon pours around the part to back off by your isolate amount. I put some underneath as well, just to make it very clear that I want no top copper under or around this part. I hope future users don't run into this problem. The new tRestrict should help. Ultimately, I hope any new eagle users can use a larger isolate. It sure helps avoid any fab house errors. On our test jigs, we usually set our isolate to 16 or sometimes 20!


    Thanks for your pina colada offer. Likewise, if you're ever in Colorado, please stop on by. Good luck with your next round of PCBs, and I hope your event goes well!